A number of companies (Radiall, Rosenberger) sell vertical surface mount SMA
connectors which we have used with blind vias to match to stripline with
very good results up to 5GHz (or 10Gbps). This is independent of board
thickness as long as you don't need more than the first and last routing
layers. I expect they would have very good matching to microstrip.

> -----Original Message-----
> From: Bob Lewandowski [SMTP:Bob.Lewandowski@Vixel.com]
> Sent: Wednesday, January 03, 2001 1:41 PM
> To: Larry Miller
> Cc: Si-List (E-mail)
> Subject: Re: [SI-LIST] : SMA test connector PCB layout
>
> Johnson Components has an "end launch" SMA that fits into a slot in the
> board edge, with a pin to contact a top surface microstrip trace. It's
> application is independent of board thickness. Johnson P/N 142-0721-88x.
> Their web site is: <http://www.johnsoncomp.com/sma.htm> A front view
> picture is shown as "End Launch". The pin diameter is 30 mils, so some
> adjustment of the launch must be made for trace widths less than 30 mils.
> Connection from the body to ground is also a significant issue with this
> type of connector. An edge plated slot that ties directly to the ground
> layers is best, both electrically and mechanically.
>
> Your other choice, the 4 ground pin through hole type is difficult to
> match to FR-4 or similar Er materials. The best possible application is
> to a back side microstrip with minimum center conductor hole and pad
> diameters. No pads on inner layers. Clear ground pads on all layers back
> as far as possible, and drill holes after plating between the center pin
> and the corner pins to reduce capacitance. With careful layout you can
> get a reflection coefficient of better than 10%.
>
> Incidentally, you should care about bad launches with a TDR because a
> large launch discontinuity masks (attenuates) downstream reflections.
>
> ---Bob Lewandowski
> Vixel Corp.
>
> Larry Miller wrote:
>
> I need to make some measurements on PC boards up to 5 GHz using a
> network
> analyzer. In the past I didn't care that much because I was doing
> TDR
> measurements.
>
> Unfortunately, the boards I will be looking at are too thick to use
> the "SMA
> edge connector" trick.
>
> Does anyone have a pointer to a good PCB footprint that will not
> have
> impedance discontinuities. The connector I want to mount is the
> familiar
> center pin + 4 ground pins vertical SMA style.
>
> Thanks in advance for any help,
>
> Larry Miller
>
> **** To unsubscribe from si-list or si-list-digest: send e-mail to
> majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
>
> si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
> si-list archives are accessible at <http://www.qsl.net/wb6tpu>
> ****
> << File: Card for Bob Lewandowski >>

**** To unsubscribe from si-list or si-list-digest: send e-mail to
majordomo@silab.eng.sun.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
****